Here is my version of the Salas Shunt Reg SSLV1.1 which I show here courtesy of Salas.
This is based on the same schematic as the one from the BiB group Buy proposed on this forum.

The spirit of this PCB is:
- As compact as possible
- Flexible Positive / negative by jumper configuration
- 1 x 22mm or 2 x 18mm electrolytics at the input + MKP bypass
- Possibility to use electrolytics to big MKP caps (I have some big 4.7uF Wima MKP10 that I want to use..) at the output
- Possibility of bypassing of sensing wires by jumper or resistor

I am looking for experts opinion, criticism and advices on the PCB layout. From general comments on the components placement, grounding, tracks routing, use of the 2 layers, etc.... basically anything that could help me make it a better design.
One thing I'm most interested in is comments on the grounding.. would I benefit from a ground plane as opposed to star grounding as it is now ? or Could I combine both ? etc..?

This is my first attempt at designing a PCB, and I know there are some (intentional) trade offs, but I am not sure of there significance so I really won't feel offended by any comment. It's open bar ...

The heatsinks are actually ON the edge... this is intentional as I believe I will use the chassis as a heatsink.... if not, I put them here just to make sure there is enough space around them and other components. I did not see the matter with the heatsinks not having PCB underneath them . But maybe I miss something ?

just some comments:
- bottom side: the connection from C5 to R1 and D2 is strange, it should be a straight connection and not go over to be so close to C1. There is very little inductive compensation you will achieve at such short runs, and the PCB inbetween
- bottom side: the GND wire that passes above C2 (upper righthand corner) is very close to that pad of C2, personally I would make that spacing wider or have the trace on top
- all traces where current is flowing should be as "rectangular" as possible, copper comes for free so just use it to widen the traces and add rectangles where they fit
- what is the purpose of having C3 and C4 sit inside each other, will one of them be stuffed from the bottom?
- agree with Piersma on the location of the heatsinks, they exist with solderable pins giving a very good mechanical connection to the PCB, so you may want to look into that.
- output GND is connected to the input caps only with one VIA at star ground, so your output current will have to pass through a smallish amount of tin inside a little hole... not ideal.. at least you may want to solder a piece of wire into this hole, to fill it with metal.
- the wires around your star ground seem all very thin. As the ground plane is on the top layer anyway, my recommendation would be to have a lot more copper on these connections.
- personally, I would do the reverse however, put a large ground plane with all the right connections on the bottom layer, and have all signal wires on the top layer, which - combined with labels - makes for much easier measuring and debugging. With designing a star ground on the PCB, you are forcing the location without real need to put it there (and not much noise improvement either), but reducing the available amount of copper to carry the current. Better to have a proper star ground at the input of your amplifier.
- no test points on your PCB. I guess that wanting to have a compact PCB leaves not much space for these (and your design is quite compact!), but they do come in handy especially for the first run

- bottom side: the connection from C5 to R1 and D2 is strange, it should be a straight connection and not go over to be so close to C1. There is very little inductive compensation you will achieve at such short runs, and the PCB inbetween

The reason is I wanted to use C5a as the ground star. and wanted to avoid creating a ground loop by going back to C5d or C5b ground. There are heavy currents flowing in the first capacitors. Not sure I understood correctly, but the technique seems to be described in Guido's paper on layout

Quote:

Originally Posted by hesener

- bottom side: the GND wire that passes above C2 (upper righthand corner) is very close to that pad of C2, personally I would make that spacing wider or have the trace on top
- all traces where current is flowing should be as "rectangular" as possible, copper comes for free so just use it to widen the traces and add rectangles where they fit

2 good points, ... modifications under way !

Quote:

Originally Posted by hesener

- what is the purpose of having C3 and C4 sit inside each other, will one of them be stuffed from the bottom?

That is to give the choice of either electrolytic OR MKT + resistor as specified by Salas in the manual. They're not intended to be used sinultaneously

Quote:

Originally Posted by hesener

- agree with Piersma on the location of the heatsinks, they exist with solderable pins giving a very good mechanical connection to the PCB, so you may want to look into that.

Yes that one made me struggle for a while.... but I decided that way as it would also increase the lead length on the FETs if I decided to bolt them on the chassis

Quote:

Originally Posted by hesener

- output GND is connected to the input caps only with one VIA at star ground, so your output current will have to pass through a smallish amount of tin inside a little hole... not ideal.. at least you may want to solder a piece of wire into this hole, to fill it with metal.

That's what I thought too.. until I realized it would be filled with the Capacitor lead and completely filled with solder anyway... but now I may want to make a few changes....

Quote:

Originally Posted by hesener

- the wires around your star ground seem all very thin. As the ground plane is on the top layer anyway, my recommendation would be to have a lot more copper on these connections.

Hmmmm and yet I did my best to put as much copper there as I could... seems that's still not enough. You're right that my strategy of placing a C there forces me to do things in a certain way, possibly not ideal..

Quote:

Originally Posted by hesener

- personally, I would do the reverse however, put a large ground plane with all the right connections on the bottom layer, and have all signal wires on the top layer, which - combined with labels - makes for much easier measuring and debugging.

Very good idea ! I'll give it a thought!! although I have to disagree on the debuging part... once all components are there it's a nightmare to track back the path of signals since you cannot see the traces anymore...

Quote:

Originally Posted by hesener

Better to have a proper star ground at the input of your amplifier.

I was planning to have a proper star ground at the input in addition to that one. Is there a problem with having little islands of stars connected together at the major star in the amp ?

Quote:

Originally Posted by hesener

- no test points on your PCB

Absolutely! and I also wanted some... my problem is just that I did not yet figure out how to create them with Eagle :P

Quote:

Originally Posted by hesener

just my two cents...

Hey , to me it's worth much more than 2 cents ! good food for thought, Thanks a lot !

Guido, Thanks a lot !
Very interesting indeed. Although I must admit, being a mechanical engineer I am lacking a lot of the background needed to understand the why's and how's ...

Also it makes me realize my search for the perfect PCB may be a little bit over engineering when I see the frequencies at play... hmmm 2.4Mhz .... all I'll be doing with that shunt reg will remain within audio frequency!